Cutting through the crust on 4140

[jderou]

I'm doing a lot of roughing on 4140 steel. The stock is 6" dia round and I am making round parts (lathe would be best I know, don't have one). I am using a 5/8 dia cobalt rougher (Tialn), running about 700 rpm at around 5-6 ipm. The crust on the outside seems to be the hardest part on the endmills, so I am trying to get around that. Right now I am spiraling from outside to inside, so the first pass around the circle is 1/2 cutter diameter into the stock, climb milling. Deepest I have run is .2", not sure if I can go much deeper or not.
Here are the options I have considered:

1. run the first pass around conventional milling, so the cutter is breaking through from the backside of the crust. Don't know what that would do.

2. Plunge through the crust just to the inside with the full cutter, then take a full width pass around just inside the crust. break/grind off outside skin remaining. Problem here is the first cut will be full diameter, not sure that would be any better for the cutter. Might have to back off on the depth also, which would make more passes, wearing out the tip of the cutter.

3. Grind off crust first. Time consuming, don't really have the best tools for the job.

Anyone have an opinion on this?

here is a pic of my setup.

[Geof]

I have used the conventional milling for the first cut approach and it seems to help a bit.

Also use carbide with air blast not coolant.

[jderou]

Would you use air blast with the cobalt also? Can't really afford to get carbide at the moment, I have 1 new cobalt left and I want to make it last.

[Geof]

Originally Posted by jderou Would you use air blast with the cobalt also? Can't really afford to get carbide at the moment, I have 1 new cobalt left and I want to make it last.

I do not think cobalt would work with just air blast. The idea with carbide and air blast is that the chip gets very hot, most of the heat stays in the chip and the workpiece and tool do not get as hot.

But!!! The cutting edge of the tool that is in direct contact with the chip and doing the work does get hot, very hot when the chip is coming off red. Carbide is quite happy with this but I do not think a cobalt tool will like it.

[HuFlungDung]

I'd say you cannot afford to not use carbide inserts on this type of job. Anywhere from $8 to $12 per insert, perhaps 2 edges per insert, it makes for relatively inexpensive roughing. For the rough cut, the inserts need not be pristine, either, and the radius corner will withstand more abuse, and possibly even a touch up 're-chamfer' of the corner if it is slightly worn or chipped. It doesn't matter if all the inserts cut the same for roughing, because, well, it's roughing.

That scale is tough on a sharp edged tool. I would recommend some brand of carbide insert mill, because inserts are commonly honed for roughing and will stand a bit of abuse. If you take the cut half width on the tool, the tool is coming down on top of the scale with very little rubbing action going on, and I think insert life will be decent. I often load up the tool with slightly used inserts for this type of rough cut, and stay near in case one blows up. Usually, carbide will give some warning with sparks being continuously generated when it is really about done for.

But, another way to try it would be helical interpolation, about 105% width of the tool. The stepdown depth can be lessened, but using the tool at full width reduces the banging effect of the cutter coming totally free of the work. If you go round in climb milling mode, the almost full width cut will have the cutting edge practically lifting the scale off from underneath. For helical interpolation, you will be making use of only the end flutes and a wee bit of the flute length.

It is possible to shorten a roughing endmill with a little bit of wear, and get 3 or 4 lives out of it. A skill well worth developing is re-gashing the end teeth, using a new endmill as a visual reference. While it is tricky to make the endmill centercutting, on a shallow ramp, only the perifery gets much use anyways. A concave grind while regashing the end teeth will suffice for a shallow ramp. Whatever you do, you must get the center 'dead zone' of the endmill away from the cutting plane. It'll glow red hot in no time if you don't.

[jderou]

I agree with you that carbide is definitely the right tool for the job. In this case I already had the roughers, so I am trying to finish the job with them. If I get more of these parts I'm going to invest in something else. Do you have much experience with solid carbide roughers compared with insert? At work we do 95% aluminum and we found we can feed a solid rougher much deeper and harder than an insert. Is this not the case for steel? Could also be a factor of machine rigidity, I couldn't come anywhere close to feeding as hard at home as at work. So maybe on a lighter machine a insert tool is a better investment?
I definitely like the cost of inserts vs a whole endmill.

[Geof]

Originally Posted by jderou .... At work we do 95% aluminum and we found we can feed a solid rougher much deeper and harder than an insert. Is this not the case for steel?...

Was this because you had problems with chips clearing from the insert cutter?

Aluminum seems to need a nice smooth path for the chips to curl out and free, I have found insert cutters don't provide adequate clearance for chips when trying to take a heavy cut.

Steel behaves differently and insert cutters often give better life and faster material removal.

[cam1]

Just 1 more perspective.....
If you are milling away the OD, why not just use a big bad angle grinder, and grind the skin off the roll,before saw cutting. It would only take a couple of minutes before the sawing operation, and the problem would be eliminated.

regards